Sameer Kulkarni

Glenn Research Center, Cleveland, Ohio

Timothy A. Beach

Coyote Hollow Consulting LLC, Walton Hills, Ohio

Gary J. Skoch

U.S. Army Research Laboratory, Glenn Research Center, Cleveland, Ohio

Computational Study of the CC3 Impeller and

Vaneless Diffuser Experiment

NASA/TM—2013-216566

September 2013

AIAA–2013–3631
NASA STI Program . . . in Profi le

Since its founding, NASA has been dedicated to the 

advancement of aeronautics and space science. The 

NASA Scientifi c and Technical Information (STI) 

program plays a key part in helping NASA maintain 

this important role.

The NASA STI Program operates under the auspices 

of the Agency Chief Information Offi cer. It collects, 

organizes, provides for archiving, and disseminates 

NASA’s STI. The NASA STI program provides access 

to the NASA Aeronautics and Space Database and 

its public interface, the NASA Technical Reports 

Server, thus providing one of the largest collections 

of aeronautical and space science STI in the world. 

Results are published in both non-NASA channels 

and by NASA in the NASA STI Report Series, which 

includes the following report types:

• TECHNICAL PUBLICATION. Reports of 

completed research or a major signifi cant phase 

of research that present the results of NASA 

programs and include extensive data or theoretical 

analysis. Includes compilations of signifi cant 

scientifi c and technical data and information 

deemed to be of continuing reference value. 

NASA counterpart of peer-reviewed formal 

professional papers but has less stringent 

limitations on manuscript length and extent of 

graphic presentations.

• TECHNICAL MEMORANDUM. Scientifi c 

and technical fi ndings that are preliminary or 

of specialized interest, e.g., quick release 

reports, working papers, and bibliographies that 

contain minimal annotation. Does not contain 

extensive analysis.

• CONTRACTOR REPORT. Scientifi c and 

technical fi ndings by NASA-sponsored 

contractors and grantees.

• CONFERENCE PUBLICATION. Collected 

papers from scientifi c and technical 

conferences, symposia, seminars, or other 

meetings sponsored or cosponsored by NASA.

• SPECIAL PUBLICATION. Scientifi c, 

technical, or historical information from 

NASA programs, projects, and missions, often 

concerned with subjects having substantial 

public interest.

• TECHNICAL TRANSLATION. Englishlanguage translations of foreign scientifi c and 

technical material pertinent to NASA’s mission.

Specialized services also include creating custom 

thesauri, building customized databases, organizing 

and publishing research results.

For more information about the NASA STI 

program, see the following:

• Access the NASA STI program home page at 

http://www.sti.nasa.gov

• E-mail your question to help@sti.nasa.gov

• Fax your question to the NASA STI 

Information Desk at 443–757–5803

• Phone the NASA STI Information Desk at

 443–757–5802

• Write to:

 STI Information Desk

 NASA Center for AeroSpace Information

 7115 Standard Drive

 Hanover, MD 21076–1320
Sameer Kulkarni

Glenn Research Center, Cleveland, Ohio

Timothy A. Beach

Coyote Hollow Consulting LLC, Walton Hills, Ohio

Gary J. Skoch

U.S. Army Research Laboratory, Glenn Research Center, Cleveland, Ohio

Computational Study of the CC3 Impeller and

Vaneless Diffuser Experiment

NASA/TM—2013-216566

September 2013

AIAA–2013–3631

National Aeronautics and

Space Administration

Glenn Research Center

Cleveland, Ohio 44135

Prepared for the

49th Joint Propulsion Conference and Exhibit

cosponsored by AIAA, ASME, SAE, and ASEE

San Jose, California, July 14–17, 2013
Acknowledgments

This effort is sponsored by the Rotary Wing Project of the NASA Fundamental Aeronautics Program. The authors acknowledge and 

thank Dr. Vikram Shyam of NASA Glenn Research Center for providing source code for the k-ω turbulence model implementation 

in TURBO and for helpful discussions. The authors would like to thank Dr. Gerard E. Welch of NASA Glenn Research Center 

and Dr. Ali Ameri of The Ohio State University for technical review of this paper and for insightful discussions. The authors also 

thank Mr. Edward P. Braunscheidel of NASA Glenn Research Center, and Dr. Wai-Ming To and Mr. Richard A. Mulac of the 

University of Toledo for numerous helpful technical discussions.

Available from

NASA Center for Aerospace Information

7115 Standard Drive

Hanover, MD 21076–1320

National Technical Information Service

5301 Shawnee Road

Alexandria, VA 22312

Available electronically at http://www.sti.nasa.gov

This work was sponsored by the Fundamental Aeronautics Program 

at the NASA Glenn Research Center.

Level of Review: This material has been technically reviewed by technical management. 
NASA/TM—2013-216566 1 

Computational Study of the CC3 Impeller and 

Vaneless Diffuser Experiment 

Sameer Kulkarni 

National Aeronautics and Space Administration 

Glenn Research Center 

Cleveland, Ohio 44135 

Timothy A. Beach 

Coyote Hollow Consulting LLC 

Walton Hills, Ohio 44146 

Gary J. Skoch 

U.S. Army Research Laboratory 

Glenn Research Center 

Cleveland, Ohio 44135 

Abstract 

Centrifugal compressors are compatible with the low exit corrected flows found in the high pressure 

compressor of turboshaft engines and may play an increasing role in turbofan engines as engine overall 

pressure ratios increase. Centrifugal compressor stages are difficult to model accurately with RANS CFD 

solvers. A computational study of the CC3 centrifugal impeller in its vaneless diffuser configuration was 

undertaken as part of an effort to understand potential causes of RANS CFD mis-prediction in these types 

of geometries. Three steady, periodic cases of the impeller and diffuser were modeled using the TURBO 

Parallel Version 4 code: (1) a k-ε turbulence model computation on a 6.8 million point grid using wall 

functions, (2) a k-ε turbulence model computation on a 14 million point grid integrating to the wall, and 

(3) a k-ω turbulence model computation on the 14 million point grid integrating to the wall. It was found 

that all three cases compared favorably to data from inlet to impeller trailing edge, but the k-ε and k-ω

computations had disparate results beyond the trailing edge and into the vaneless diffuser. A large region 

of reversed flow was observed in the k-ε computations which extended from 70 to 100 percent span at the 

exit rating plane, whereas the k-ω computation had reversed flow from 95 to 100 percent span. Compared 

to experimental data at near-peak-efficiency, the reversed flow region in the k-ε case resulted in an underprediction in adiabatic efficiency of 8.3 points, whereas the k-ω case was 1.2 points lower in efficiency. 

Nomenclature 

CFD computational fluid dynamics 

CMOTT Center for Modeling of Turbulence and Transition 

k turbulence kinetic energy (TKE) 

R radius 

RTE radius of impeller trailing edge (215.5 mm) 

RANS Reynolds-averaged Navier Stokes equations 

y+

 dimensionless wall distance 

ε dissipation of turbulence kinetic energy 

ω specific turbulence dissipation 
NASA/TM—2013-216566 2 

Introduction 

Centrifugal compressors are frequently used in the high pressure compressor of turboshaft engines 

due to the low exit corrected flow rates in these machines. With the decreasing size of the high pressure 

compressor in turbofan engines as engine overall pressure increases, exit corrected flow rates may be 

sufficiently low such that the use of a centrifugal stage at the compressor exit may provide performance 

benefits over a typical axial compressor stage (Ref. 1). Thus, the ability to accurately simulate the flow 

within centrifugal stages is becoming increasingly important for compressor designers and researchers. 

However, Reynolds-averaged Navier-Stokes (RANS)-based computational fluid dynamics (CFD) results 

published in the literature tend to mis-predict the performance of centrifugal compressors when compared 

to available data (Refs. 2 to 5). In general, the computations tend to over-predict total pressure ratio, 

efficiency, and in the case of vaned diffuser configurations, the choking flow rate. 

The current research effort was undertaken in an attempt to investigate and understand the potential 

causes of the mis-prediction of centrifugal compressor impeller performance by RANS solvers. Figure 1 

shows the impeller studied in this investigation, a centrifugal compressor known as CC3. This test 

compressor is a 4.54 kg/s (10 lbm/s) machine which was scaled up from a 1.658 kg/s (3.655 lbm/s) Allison 

Engine design. The design exit corrected flow rate of the test compressor is 1.36 kg/s (3.0 lbm/s). The 

complete design description and hot shape geometry of the test compressor are given by McKain and 

Holbrook (Ref. 6). The test compressor was used in aerodynamics studies at NASA Glenn Research 

Center (Refs. 7 to 9). The impeller was tested in both vaned diffuser and vaneless diffuser configurations, 

and detailed measurements of the flow field were obtained. The data available for this test compressor 

qualifies it as a good candidate for further computational studies. 

The CFD solver used in the current work is the TURBO Parallel Version 4 code. TURBO is a threedimensional, viscous, unsteady RANS solver for turbomachinery flows. Flux vector splitting is used in 

evaluating flux Jacobians on the left hand side, while Roe’s flux difference splitting is used to form a 

higher order TVD scheme for convective fluxes on the right hand side. The code can use multiple 

structured blocks with matching boundaries. Local time stepping can be employed to accelerate 

convergence for steady-state flows. Newton sub-iterations are applied to unsteady flows to obtain a 

converged solution within each time step (Ref. 10). Multiple blade rows can be modeled with sector 

periodic blade row meshes using a simple periodic boundary condition or with a single blade passage per 

blade row using phase lag boundary conditions (Refs. 11 and 12). The default turbulence model in 

TURBO is the NASA/CMOTT k-ε turbulence model with wall functions (Ref. 13). The code has 

previously been validated on various geometries (Refs. 14 and 15). 

Figure 1.—CC3 impeller and vaned diffuser hardware (Ref. 9). 
NASA/TM—2013-216566 3 

 As a precursor to the current research effort, unsteady phase-lag simulations of the CC3 impeller with 

the vaned diffuser configuration were generated using TURBO. The resulting speed line at the design 

speed is shown in Figure 2 alongside a comparison to the data. An over-prediction in choking flow rate 

was observed in the CFD result, and this speed line serves to illustrate a trend seen throughout the 

literature (Refs. 2 to 5). 

 The CFD results shown are converged, unsteady phase-lag computations which were time-averaged 

over one revolution. Computed static pressures at the exit rating station were area-averaged. In these 

simulations, a grid of 4.3 million points with resolution deemed to be typical of turbomachinery CFD was 

used. A row of three support struts upstream of the impeller, as well as leakage flows, were neglected in 

the computation. The computation over-predicted pressure ratio by 3.3 percent at the design point inlet 

corrected flow rate (shown as a filled symbol) and over-predicted choking flow rate by 1.9 percent. The 

computation was run with ambient inlet pressure of 101,325 Pa, whereas the data was taken at 

approximately 86,000 Pa. The computation was performed with the measured clearances, which are 

minimum tip clearances. If clearances are highly non-axisymmetric in the test article, modeling the 

minimum tip clearance may explain part of the over-prediction in the computed performance. The 

questions of clearance sensitivity and Reynolds number sensitivity are left for future work. Instead, it was 

hypothesized that the over-prediction of performance may be due to inaccurate simulation of the 

unsteady, non-uniform impeller discharge flow and the subsequent impact on associated time-mean 

aerodynamic blockage at the diffuser throat. 

 The scope of the research effort was narrowed to more closely examine the impeller exit flow. The 

focus of this paper is the CC3 impeller in its vaneless diffuser configuration. The compressor was 

modeled as a steady, periodic, single blade row computation in TURBO, which reduced computational 

expense and run-times. While the vaneless configuration obviates the impact of periodic unsteadiness, it 

was anticipated that lessons learned in modeling this simpler case may be useful in future work involving 

impellers and vaned diffuser configurations. The details of the compressor experiments are provided in 

the next section, followed by details of the computational effort. 

Figure 2.—Computed and experimental total-to-static 

pressure ratios of CC3 vaned diffuser configuration 

at design speed. 

2.5

2.7

2.9

3.1

3.3

3.5

3.7

3.9

4.1

4.3

4.5

9 9.5 10 10.5 11

Total‐to‐Static Pressure Ratio

Inlet Corrected Flow (lbm/s)

Data

TURBO
NASA/TM—2013-216566 4 

Details of the Experiment 

 The focus of the current work was the CC3 impeller in its vaneless diffuser configuration. A 

cross-section of the compressor rig is shown in Figure 3. Table 1 summarizes important design 

parameters. The impeller consists of 15 main blades and 15 splitter blades having 50 of backsweep from 

the radial direction. The design corrected speed was 21,789 rpm, and the measured minimum clearances 

at this speed were 0.1524 mm (0.006 in.) at the leading edge, 0.6096 mm (0.024 in.) at the midchord 

“knee” and 0.2032 mm (0.008 in.) at the trailing edge (Ref. 7). At this clearance schedule and in the cold 

shape, the impeller hub at the trailing edge sat axially forward of the diffuser hub by 0.127±0.0508 mm 

(0.005±0.002 in.). This step in the hub was neglected in the computations. 

Total pressure and total temperature exit rakes were located at eight evenly spaced circumferential 

locations at radius ratio R/RTE = 1.18. Each total pressure rake had four elements located at 19.2, 43.4, 

68.2, and 93.1 percent of span, and each total temperature rake had three elements located at 23.1, 55.9, 

and 88.9 percent of span. Performance parameters were calculated using arithmetic averages of these rake 

elements. An inlet probe was used to acquire spanwise total pressure at a station 2.54 cm (1.0 in.) 

upstream of the impeller main blade leading edge (Fig. 4). Spanwise total pressure surveys were also 

acquired by using a constant-blockage probe immersed downstream of the impeller trailing edge at radius 

ratio R/RTE = 1.10. Features which were neglected in the computations include a row of three inlet struts 

upstream of the impeller, impeller blade fillets, and backplate leakage paths. A set of 16 equally spaced 

5/16th in. diameter pins, which held together the diffuser hub and shroud, were located in the test 

compressor at radius ratio R/RTE = 1.45. These structural elements were thought to be sufficiently far 

downstream of the exit rating station and were neglected in the computational model. 

Figure 3.—Cross-sectional drawing of the CC3 rig in the 

vaneless diffuser configuration (Ref. 7). A is the exit 

rating station, R/RTE = 1.18; B is the impeller main 

blade leading edge; C is the impeller splitter blade 

leading edge; D is the leading edge of a row of support 

struts; E is the impeller trailing edge. 

Figure 4.—CC3 inlet survey data measured 2.54 cm 

(1.0 in.) upstream of impeller leading edge.

TABLE 1.—CC3 IMPELLER DESIGN PARAMETERS 

Impeller main blade count 15 

Impeller splitter blade count 15 

Design corrected speed 21,789 rpm 

Design inlet corrected flow rate 4.54 kg/s 

Design exit corrected flow rate 1.36 kg/s 

Impeller exit tip speed 492 m/s 

Inlet blade height 64 mm 

Exit blade height 17 mm 

Leading edge tip radius 105 mm 

Trailing edge radius, RTE 215.5 mm 

Impeller backsweep 50° 

0

0.2

0.4

0.6

0.8

1

0.96 0.97 0.98 0.99 1 1.01

Fraction Span

Total Pressure Ratio
NASA/TM—2013-216566 5 

Details of the Computations 

The default turbulence model in TURBO Parallel Version 4 is the NASA/CMOTT k-ε model with 

wall functions (Ref. 13). In addition to the default k-ε model, Wilcox’s k-ω turbulence model was used 

(Ref. 16). The implementation of the k-ω model does not include wall functions, and the k-ω model 

required a grid with sufficiently low y+

 so as to allow integration to the wall. Thus, two different grids 

were used in the current effort. A “baseline” grid with approximately 6.8 million points and y+

 on the 

order of 50 was used for k-ε computations with wall functions enabled. A “refined” grid containing 

approximately 14 million points was also generated, allowing integration to the wall for k-ω as well as k-ε

computations, in an effort to characterize the effect of varying grid resolution on aerodynamic 

performance. A histogram of y+

 for the k-ε and k-ω computations on the refined grid is shown in Figure 5. 

Typically, y+

 was less than 3 for a majority of the walls. Values of y+ approached 5 along the blunt 

trailing edge of the impeller and at the shroud near the trailing edge of the suction side of the impeller, but 

these were within the viscous sublayer region. In all computational cases, inlet turbulence intensity was 

set to 1 percent, and inlet turbulent eddy viscosity ratio was set to 100.0. These values correspond to an 

inlet turbulence length scale of approximately 0.6 percent of the impeller inlet blade height. 

TURBO solves the unsteady RANS equations on multiblock structured grids. All grids, boundary 

condition files, and block connectivity files for TURBO were generated using the Turbomachinery 

Gridding System (TGS) (Ref. 17). The measured tip clearances, which were minimum tip clearances, 

were included in the computational grid. Impeller blades and tip clearances were gridded with O-blocks, 

and H-blocks were used to connect the O-blocks around the impeller main and splitter blades. The block 

topology of the refined grid is shown in Figure 6. The computational domain consists of the axial inlet, an 

impeller and splitter passage, the vaneless diffuser, and the S-bend to the axial outlet. A meridional view 

of the computed flow path is shown in Figure 7. 

Steady, single passage periodic simulations were converged at design speed using local time stepping. 

Solid walls were modeled with no-slip boundary conditions and were assumed to be adiabatic. The 

specific heat coefficient ratio was assumed constant. The inlet boundary condition was specified with 

spanwise profiles of total pressure, total temperature, radial flow angle, and tangential flow angle. The 

total pressure profile, shown in Figure 4, was the measured inlet probe survey data from the CC3 

experiment. The computations were referenced to an inlet pressure of 101,325 Pa, whereas the data was 

taken at reduced inlet pressures on the order of 85,500 Pa. Inlet total temperature was assumed constant 

288.15 K, and zero inlet tangential flow angle was assumed. The profile of inlet radial flow angle was 

found by linear interpolation between the geometry angles of the hub and shroud at the inlet. The 

computations were throttled from choke, up the speed line, but were not taken to the stall boundary. The 

operating point was set by using a radial equilibrium exit boundary condition, specifying exit static 

pressure at the shroud. 

Figure 5.—Histogram comparing y+ of k-ε and k-ω

computations on the refined grid near design point. 

0

20

40

60

80

100

0.25 1.75 3.25 4.75 6.25 7.75 9.25 10.75

Number of Cells (in thousands)

y+

Refined k‐epsilon

Refined k‐omega
NASA/TM—2013-216566 6 

Figure 6.—Block topology of the CC3 impeller and 

vaneless diffuser.

Figure 7. —Meridional view of the CC3 impeller and 

vaneless diffuser model. 

Results 

Design speed computations of the impeller and vaneless diffuser were generated using TURBO. 

Three computed speed lines are compared to data in Figure 8. The three computed results are the k-ε

result with wall functions on the baseline grid, and the k-ε and k-ω results integrating to the wall on the 

refined grid. The computations were not taken to the stall boundary or deep into choke, as comparisons to 

the near-peak-efficiency data point were of interest in the current effort. The computed results were areaaveraged in the circumferential direction at the exit rating station location, R/RTE = 1.18. The areaaveraging of the steady computations in the rotating frame of reference is analogous to the time-averaging 

done by the steady rake instrumentation, which is fixed in the stationary frame of reference while 

immersed in the unsteady rotor exit flow. The circumferential averaging yielded a spanwise profile of 

computed total pressure and total temperature. An arithmetic average of the values of total pressure and 

total temperature at those spanwise locations which correspond to the rake element locations was 

calculated, which was analogous to the experimental averaging approach. 

The choking flow rates of the baseline and refined k-ε computations agree to within 0.33 percent of 

each other. The k-ω computation choked at corrected flow 0.5 percent lower than the refined k-ε

computation. This difference is attributed to a slightly larger growth in the boundary layer in the k-ω

result along the pressure side of the main impeller blade. The larger boundary layer results in increased 

aerodynamic blockage, reducing both effective flow area and choking flow rate. The k-ω computation 

under-predicts choking flow rate by 1.22 percent as compared to data. 

Both k-ε results under-predict total pressure ratio and efficiency as compared to the data. The k-ω

computations better match the data on these performance parameters. The near-peak-efficiency data point 

and the computed operating points at nearby inlet corrected flow rates are shown as filled symbols in 

Figure 8. These operating points were compared. All three sets of computations over-predicted the work 

done by the impeller, as shown by the total temperature curves which are approximately 0.6 percent 

higher than the data. Compared to the near-peak-efficiency data point, the baseline k-ε result was 

7.2 points lower in efficiency and 7 percent lower in total pressure ratio. The refined k-ε result was 

8.3 points lower in efficiency and 8 percent lower in total pressure ratio than the data. The k-ω result was 

1.2 points lower in efficiency and 0.6 percent higher in total pressure ratio than the data. In this case, the 

choice of turbulence model evidently had a much greater impact on the flow field than the selected level 

of grid density. 

Exit rating station,

R/RTE=1.18

Impeller trailing edge, 

R/RTE=1.00 

Splitter leading edge

Impeller 

leading edge 
NASA/TM—2013-216566 7 

A comparison of shroud static pressures at these operating points is shown in Figure 9. The data have 

been normalized by the plenum pressure of 85,360 Pa and the computations are referenced to inlet total 

pressure 101,325 Pa. The shroud static pressures of the data, the k-ω case, and both k-ε cases show very 

good agreement from the inlet to the impeller trailing edge. Downstream of the trailing edge, the baseline 

and refined k-ε computations have virtually identical shroud static pressures. The k-ε computations have 

reduced pressure recovery through the diffuser as compared to the data and to the k-ω computation. In the 

vaneless diffuser, the k-ω simulation matches the data well through the initial half of the diffuser, but 

over-predicts pressure recovery towards the S-bend and beyond. 

Figure 8.—Total pressure ratio, total temperature ratio, and adiabatic efficiency of CC3 vaneless diffuser configuration 

at design speed. Note: the computed speed lines were not run to stall. 

3.1

3.3

3.5

3.7

3.9

4.1

4.3

4.5

Total Pressure Ratio

Data Baseline k‐epsilon

Refined k‐epsilon Refined k‐omega

1.5

1.52

1.54

1.56

1.58

1.6

1.62

1.64

1.66

Total Temperature Ratio

Data Baseline k‐epsilon

Refined k‐epsilon Refined k‐omega

7 7.5 8 8.5 9 9.5 10 10.5 11 11.5 12

70

72

74

76

78

80

82

84

86

88

Inlet Corrected Flow (lbm/s)

Adiabatic Efficiency

Data Baseline k‐epsilon

Refined k‐epsilon Refined k‐omega
NASA/TM—2013-216566 8 

Figure 9.—Computed and experimental static pressure ratio along the shroud surface. Vertical lines mark geometry 

features of interest. 

In Figure 10 spanwise profiles of the computed flow angles (from tangential) and total pressures are 

compared against the profiles measured by the constant-blockage probe at radius ratio R/RTE = 1.10. This 

is a location nearly midway between the impeller trailing edge and the exit rating station, where the 

shroud static pressures of the k-ω case and the k-ε cases are diverging. The uncertainty of the measured 

flow angle is not obvious, so measured flow angles are shown with both ±1° and ±3° error bars for 

reference. The comparison shows that the baseline and refined k-ε computations both yield nearly 

identical total pressure and tangential flow angle profiles. The flow angle profiles indicate that the k-ε

computations have a region of reversed flow (i.e., negative tangential flow angle) in the top 25 percent of 

the passage. This large region of reversed flow is an aerodynamic blockage which causes higher velocities 

and thus higher flow angles in the bottom 75 percent of the passage, as compared to the data. The 

reversed flow near the shroud is evidently the cause of the large deficit in total pressure observed in the 

k-ε computations, which disagree with the measured pressure profile above 55 percent span. The data 

indicates reversed flow within the top 10 to 15 percent of span near the shroud. The flow angle profile 

from the k-ω computation agrees with the data in this regard. The k-ω computation over-predicts flow 

angle in the bottom 50 percent of span, but to less of a degree than either k-ε computation. The k-ω

computation misses the pressure deficit seen in the survey data above 75 percent span. 

In Figure 11, a comparison of flow angles is made between the three computations at two locations; 

just downstream of the trailing edge (R/RTE = 1.01), where the shroud static pressures are in agreement, 

and at the exit rating station (R/RTE = 1.18), where there is a large difference in shroud static pressures. 

The flow angle profiles of the three computations match well near the trailing edge. At R/RTE = 1.01, the 

flow angle profiles of the k-ε cases match each other to within ±0.5°, and the k-ω case matches the k-ε

cases within ±1.5°, with slight disagreement above 95 percent span. The k-ε cases indicate reversed flow 

beginning at 97 percent span, the k-ω case indicates reversed flow at 95 percent span. There is large 

disparity between the k-ε cases and the k-ω case at radius ratio R/RTE = 1.18. The flow angle profiles of 

the two k-ε computations, which agree to within ±1.0°, indicate that the flow has reversed in nearly 

30 percent of the span near the shroud. The k-ω case has reversed flow in only the upper 5 percent of span 

near the shroud. 

0.5

1

1.5

2

2.5

3

3.5

4

0 10 20 30 40 50 60 70 80 90 100

Shroud Static Pressure Ratio

Shroud Arc Length (%)

Data

Baseline k‐epsilon

Refined k‐epsilon

Refined k‐omega
NASA/TM—2013-216566 9 

Figure 10.—Area-averaged computed total pressure ratio (left) and flow angle (right) compared to survey data at 

radius ratio R/RTE = 1.10. 

0

0.1

0.2

0.3

0.4

0.5

0.6

0.7

0.8

0.9

1

2.00 3.00 4.00 5.00

Fraction Span

Total Pressure Ratio

Data

Baseline k‐epsilon

Refined k‐epsilon

Refined k‐omega

‐20.00 ‐10.00 0.00 10.00 20.00 30.00

Flow Angle (deg) from Tangential

Data

Baseline k‐epsilon

Refined k‐epsilon

Refined k‐omega

Figure 11.—Area-averaged flow angles comparing results of the k-ε and k-ω turbulence models at radius ratios 

R/RTE = 1.01 (left) and R/RTE = 1.18 (right). 

0

0.1

0.2

0.3

0.4

0.5

0.6

0.7

0.8

0.9

1

‐10 0 10 20 30

Fraction Span

Tangential Flow Angle (deg)

Flow Angle Profile at R/RTE = 1.01

Baseline k‐epsilon

Refined k‐epsilon

Refined k‐omega

0

0.1

0.2

0.3

0.4

0.5

0.6

0.7

0.8

0.9

1

‐40 ‐20 0 20 40

Fraction Span

Tangential Flow Angle (deg)

Flow Angle Profile at R/RTE = 1.18

Baseline k‐epsilon

Refined k‐epsilon

Refined k‐omega
NASA/TM—2013-216566 10 

Figure 12. —Radial velocity contours (normalized by 287.6 m/s) at the trailing edge of the impeller, R/RTE = 1.01 (left), 

and at the exit rating station R/RTE = 1.18 (right). Impeller blade rotation is right-to-left. 

The deficit in static pressure recovery seen in the k-ε computations is attributed to the large region of 

reversed flow. This region is shown in Figure 12, which plots the computed radial velocity contours near 

the impeller trailing edge, R/RTE = 1.01, and at the exit rating station, R/RTE = 1.18. The contours near the 

trailing edge show the splitter blade in the middle of the plot, and the main blade at the left and right sides 

of the plot. At R/RTE = 1.01, the low-momentum regions near the hub that extend into mid-span are 

associated with the impeller blade wakes. The low radial velocity region at the shroud is the tip clearance 

flow. The spanwise extent of the clearance flow is slightly larger in the k-ε computations as compared to 

the k-ω computation, indicating a stronger tip clearance vortex in the k-ε computations. The flow fields of 

the two different turbulence models are qualitatively and quantitatively similar at the trailing edge. If 

performance is computed from the inlet plane to the plane defined by R/RTE = 1.01, the refined k-ε and 

k-ω computations agree to within 0.7 percent in total pressure ratio and to within 1.0 point in adiabatic 

efficiency. At the exit rating station R/RTE = 1.18, the two k-ε computations are qualitatively very 

different from the k-ω computation, and the computed performance parameters at R/RTE = 1.18 amount to 

a 8.4 percent difference in total pressure ratio and 7.0 point difference in adiabatic efficiency between the 

refined k-ε and k-ω computations. 

Figure 13 plots entropy on planes of constant radius through the last 30 percent of impeller chord to 

show loss development through the passage. In the figure, the pressure side of the main blade is on the 

right, the splitter blade is in the middle, and the suction side of the main blade is on the left. The 

computations differ at the corner formed by the pressure side of the main blade and the shroud. The 

higher magnitude of entropy in the refined k-ε case indicates larger loss due to a stronger tip clearance 

flow than in the baseline k-ε case. The spanwise extent of the high entropy region is smaller in the k-ω

case, indicating a weaker tip clearance flow than in the k-ε cases. Qualitatively, the entropy contours 

among the three computations are similar through the trailing edge. 

   ROTATION
NASA/TM—2013-216566 11 

Figure 13.—Entropy contours at constant-radius planes over the last 30 percent of impeller chord, with the splitter 

blade shown in the center of the passage. 

Figure 14 plots radial velocity through the radial diffuser and axial velocity after the S-bend. These 

velocities were area-averaged in the circumferential direction for the k-ε and k-ω results on the refined 

grid. This shows the extent of the reversed flow through the diffuser along the shroud in each case. In 

both computations, the impeller exit flow is similar, but differences arise in the diffuser. Both computations show reversed flow at the shroud at close proximity to the impeller trailing edge. In the k-ε

Figure 14. —Area-averaged velocity contours (normalized by 

287.6 m/s) showing streamwise components (radial component 

in the radial diffuser and axial component after the radial-toaxial S-bend). 

ROTATION
NASA/TM—2013-216566 12 

computation, the reversed flow persists up the radius of the diffuser along the shroud surface. In the k-ω

case, there is a relatively small bubble of reversed flow which weakens as radius increases through the 

diffuser. The separated region in the k-ε cases reattaches through the S-bend and there is no negative axial 

velocity at the end of the computational domain. The diffuser flow field had large sensitivity upon the 

choice of turbulence model. A discussion on the differences in the diffuser flow field is presented next, as 

well as comments and suggestions for future work. 

Discussion 

 A better understanding of the cause of the disparate diffuser flow fields between the k-ε and k-ω

computations is of interest for future work. The flow fields indicate that the k-ω computation has greater 

turbulent mixing in the diffuser, which causes the shroud separation to weaken and mix out in a manner 

that is not occurring in the k-ε computations. Figure 15 shows a band of high turbulence kinetic energy 

(TKE) in the diffuser of the k-ε case which is not evident in the k-ω case. This region is attributed to the 

shear layer at approximately 70 percent span due to the interface of the separated flow and core flow in 

the k-ε case. Generally, it was observed in the k-ω computation that the levels of both production and 

dissipation of TKE were higher than the k-ε computations near the shroud within the impeller passage, 

but these terms were lower than the k-ε computations through the diffuser. 

It may be of interest in future work to generate a simulation using a standard k-ε model, which sets 

constant Cμ = 0.09 in the turbulent eddy viscosity equation rather than a computed value as in the 

CMOTT k-ε model. As shown in Figure 16, the computed Cμ in the refined CMOTT k-ε result yields 

values lower than 0.09 in the shear layer region at 70 percent span in the diffuser at the exit rating station. 

A standard k-ε model would increase Cμ in this region, resulting in increased turbulent eddy viscosity and 

turbulent mixing, which may mix out or weaken the separation observed in the current k-ε cases. 

Figure 15.—Turbulence kinetic energy at constant-radius planes from R/RTE = 0.9 to R/RTE = 1.18. The splitter blade 

is shown in the center of the passage. 
NASA/TM—2013-216566 13 

The current results suggest that the flow developing through the radial diffuser may largely depend on 

the selection of turbulence model. In a vaned diffuser configuration, a strong separation entering the 

diffuser impacts the aerodynamic blockage, which affects the pressure rise and flow capacity in the 

diffuser. The impact of different turbulence models on this separation, and thus on the stage performance, 

should be analyzed in future work. The vaned diffuser computation poses a more complicated problem, as 

the blockage will also be dependent upon the unsteadiness due to the impeller/vane interaction in a vaned 

diffuser configuration. 

Conclusion 

A computational study of the CC3 impeller in its vaneless diffuser configuration was undertaken. 

TURBO CFD simulations were generated on: (1) a baseline grid using the default CMOTT k-ε turbulence 

model, (2) a refined grid using the default CMOTT k-ε turbulence model, and (3) a refined grid using 

Wilcox’s k-ω turbulence model. The results indicated that all three computational cases matched the data 

well from the inlet, through the impeller, and up to the trailing edge. The area-averaged flow angle 

profiles of the baseline and refined k-ε cases matched to within ±0.5° just downstream of the impeller 

trailing edge (R/RTE = 1.01). At this radius ratio, the flow angle profile of the k-ω case matched both k-ε

cases to within ±1.5°, and the refined k-ε and k-ω computations agreed to within 0.7 percent in total 

pressure ratio and to within 1.0 point in adiabatic efficiency. Beyond the trailing edge and into the 

diffuser, the k-ω computation continued to match the data, but the k-ε computations yielded pressure and 

efficiency deficits as compared to data due to a large reversed flow region extending from the shroud 

surface of the vaneless diffuser. At the experimental exit rating station (R/RTE = 1.18), the baseline k-ε

computation is 7.2 points lower in efficiency and 7 percent lower in total pressure ratio than the data. The 

refined k-ε computation is 8.3 points lower in efficiency and 8 percent lower in total pressure ratio than 

the data. The k-ω computation is 1.2 points lower in efficiency and 0.6 percent higher in total pressure 

ratio than the data. It was shown that the potential impact of the choice of turbulence model may be quite 

large on the diffuser flow field. 

References 

1. Welch, G.E., Hathaway, M.D., Skoch, G.J., Snyder, C.A., “Rotary-wing relevant compressor aero 

research and technology development activities at Glenn Research Center,” NASA TM-217280, 

2012. 

2. Chen, J.P., Webster, R.S., Hathaway, M.D., Herrick, G.P., and Skoch, G.J., “Numerical Simulation of 

Stall and Stall Control in Axial and Radial Compressors,” AIAA Paper No. AIAA-2006-418, 2006. 

3. Lurie, E.A., Van Slooten, P.R., Medic, G., Mulugeta, M.M., Holley, B.M., Feng, J., Sharma, O., and 

Ni, R., “Design of a High Efficiency Compact Centrifugal Compressor for Rotorcraft Applications,” 

American Helicopter Society 67th Forum, 2011. 

4. Smythe, C.J., “Forced Response Predictions in Modern Centrifugal Compressor Design,” M.S. 

Thesis, Department of Aeronautics and Astronautics, Massachusetts Institute of Technology, 2005. 

Figure 16. —Cμ of the refined grid k-ε computation at 

radius ratio R/RTE = 1.18 (exit rating station).
NASA/TM—2013-216566 14 

5. Tarr, D.L., “Scaling of Impeller Response to Impeller-Diffuser Interactions in Centrifugal 

Compressors,” M.S. Thesis, Department of Aeronautics and Astronautics, Massachusetts Institute of 

Technology, 2008. 

6. McKain, T.F., and Holbrook, G.J., “Coordinates for a High Performance 4:1 Pressure Ratio 

Centrifugal Compressor,” NASA CR-204134, 1997. 

7. Skoch, G.J., Prahst, P.S., Wernet, M.P., Wood, J.R., and Strazisar, A.J., “Laser Anemometer 

Measurements of the Flow Field in a 4:1 Pressure Ratio Centrifugal Impeller,” ASME Turbo Expo, 

Paper No. 97-GT-342, 1997. 

8. Wernet, M.P., Bright, M.M., and Skoch, G.J., “An Investigation of Surge in a High-Speed Centrifugal 

Compressor Using Digital PIV,” J. Turbomachinery, Vol. 123, Apr. 2001, pp. 418-218. 

9. Larosiliere, L.M., Skoch, G.J., and Prahst, P.S., “Aerodynamic Synthesis of a Centrifugal Impeller 

Using Computational Fluid Dynamics and Measurement,” J. Propulsion and Power, Volume 15, 

Number 5, 1999, pp. 623-632. 

10. Chen, J.P., and Whitfield, D.L., “ Navier-Stokes Calculations for the Unsteady Flowfield of 

Turbomachinery,” AIAA Paper No. AIAA-93-0676, 1993. 

11. Chen, J.P., and Barter, J., “Comparison of Time-Accurate Calculations for the Unsteady Interaction in 

Turbomachinery Stages,” AIAA Paper No. AIAA-98-3293, 1998. 

12. Chen, J.P., and Briley, W.R., “A Parallel Flow Solver for Unsteady Multiple Blade Row 

Turbomachinery Simulations,” ASME Turbo Expo, Paper No. 2001-GT-0348, 2001. 

13. Zhu, J., and Shih, T.H., “CMOTT Turbulence Module for NPARC,” NASA CR-204143, 1997. 

14. Turner, M. G., “Multistage Turbine Simulations with Vortex-Blade Interaction,” Journal of 

Turbomachinery, Vol. 118, Oct. 1996, pp. 643–653. 

15. Van Zante, D.E., To, W., and Chen, J.P., “Blade Row Interaction Effects on the Performance of a 

Moderately Loaded NASA Transonic Compressor Stage,” ASME Paper GT-2002-30575, 2002. 

16. Shyam, V., Ameri, A., and Chen, J.P., “Validation of Heat Transfer and Film Cooling Capabilities of 

the 3-D RANS Code TURBO,” NASA TM-216738, 2010. 

17. Beach, T.A., “Centrifugal Compressor Analysis using the TURBO Flow Solver,” NASA CR to be 

published, 2013.